section lining

[dakeb]

I would like to display a section through a gear. Drawing standards dictate the gear teeth should not be hatched (section lined) even though the cutting plane passes through them. I have the same problem with sections through webs.

Is there a way in UG of displaying these sectional views in accordance with drawing standards?

 

[cowski]

Would it work to just turn off the hatching for the gear? Is this a section through an assembly (multiple parts) or just the gear?

Or do you need to hatch through the hub but not the teeth? If that is the case, you could turn off the hatching and define your own boundary to hatch (not elegant but it works).

 

[fgbrender]

I agree with cowski. There is another option when you want some components hatched while others are not. Simply move the hatching you don't wish to see to an invisible layer. Not sure if you can apply hatching to some components and not others. Looking into it.

 

[looslib]

There is an attribute that can be put into part files so that they will not show section lines when the part is cut by the cutting plane of the section.

Don't have access the documentation to find it, but it is something like: section_view = no.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
Sr IS Technologist
L-3 Communications

 

[cowski]

You can selectively hatch components in a view with 'section components in view' (in NX2 it is in Edit -> View -> Section components in view...). I have only used it once or twice so if it sounds useful I would suggest hitting the help file.

 

[fgbrender]

Looslib,
If I'm following you correctly, what you describe determines whether or not the section lines are shown in the parent view. It's a checkbox in the dialog for creating the section view.

Cowski,
I have used "section components in view" quite a lot. What it does is defines which components are actually cut in the section view. Unfortunatly does not control hatching of components.

I'm not familiar with nor have I found any way to apply hatching to only select components. I've checked the documentation and the only thing I can find is the checkbox in the Style dialog.

 

[cowski]

fgbrender,
Thanks for the correction to my post.

 

[looslib]

No it is not a check box.
We had a part attribute that we added to our hardware items that would prevent them from being hatched when they were cut with a cutting plane for a section.

This is from the V17 Drafting documentation:
Creating non-sectioned components

Component parts added to an assembly, by default, are sectioned in section views on the assembly part drawing. You can make the components non-sectioned, by setting the user-defined part attribute section-component as follows:

Make the component part the work part.

Choose Format—>Attribute—>Part.

Choose Assign.

Enter section-component as the title for the String Attribute and choose OK.

Enter no as the String Value and choose OK.

Choose OK to dismiss the Enter Title For String Attr dialog.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
Sr IS Technologist
L-3 Communications

 

[PennKoff]

dakeb,

Have you tried Edit?Crosshatch Boundary? It's pretty well covered in the help files. Does this solve your problem or am I missing something?

_____________________________________
"Complex problems have simple, easy-to-understand, wrong answers."
_________________
PI Penkov
CAM Programmer
Non-standard Equipment Designer

 

[dakeb]

This is a drawing of a single component, not an assembly, and the section cut through the component needs to be only partially crosshatched to comply with drawing standards. I don't think you can edit automatically generated crosshatch boundaries of section views. Looks like one way to do it is to suppress the automatic crosshatching and define a boundary manually, as suggested by others.

 

[PennKoff]

Just try Edit->Crosshatch Boundary. Of course you can edit the boundary of automatically generated crosshatch:

_____________________________________
"Complex problems have simple, easy-to-understand, wrong answers."
_________________
PI Penkov
CAM Programmer
Non-standard Equipment Designer

 

[dakeb]

How do you create the new boundary? Inserting curves on the drawing don't seem to work.

 

[PennKoff]

I simply follow these steps:

1. expand the member view
2. sketch the boundary needed to be included
3. switch off expanding the view
4. edit->crosshatch boundary
5. choose "Add" option
6. select the crosshatch
7. select the boundary
8. hit "apply" or "update crosshatch"

Does this help?

_____________________________________
"Complex problems have simple, easy-to-understand, wrong answers."
_________________
PI Penkov
CAM Programmer
Non-standard Equipment Designer

 

[fgbrender]

looslib,
Sorry, I misunderstood your post. I thought you were talking about turning off section lines in your original post. What you describe in your last post is setting a component to not be sectioned. This can be accomplished by using Edit -> View -> Section components in view. I was not aware this could also be done with an attribute.

PennKoff,
Looks like an good solution.

 

[looslib]

The advantage of the attribute is you can define it for all of your hardware items and the section hatching is off automatically in assemblies, no additional commands and component picking needed.
Since our hardware parts were generated from a master file, we put the attribute in that file and all new hardware files had the attribute when they were created.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
Sr IS Technologist
L-3 Communications

 

[PennKoff]

fgbrender,

Yes, it's a good one. I believe that's the job dakeb wanted to do. I'm not fluent in english.

_____________________________________
"Complex problems have simple, easy-to-understand, wrong answers."
_________________
PI Penkov
CAM Programmer
Non-standard Equipment Designer